HEIDENHAIN SW 54843x-02 DIN Programming - Manual (Page 315)

HEIDENHAIN MANUALplus 620, CNC PILOT 640 315
4.22 Dr
illing cy
cles
Boring, countersinking G72
G72 is used for holes with contour definition (individual hole or hole
pattern). Use G72 for the following axial and radial drilling functions
using driven or stationary tools:
 Boring
 Countersinking
 Reaming
 NC drilling
 Centering
Parameters
ID
Drilling contour—Name of the hole definition
NS Block number of contour. Reference to the contour of the hole
(G49-Geo, G300-Geo or G310-Geo)
E Period of dwell for chip breaking at end of hole (in seconds)—
(default: 0)
D Retraction type (default: 0)
 0: Rapid traverse
 1: Feed rate
BS Start element no. (number of the first hole to be machined in a
pattern)
BE End element no. (number of the last hole to be machined in a
pattern)
H (Spindle) Brake off (default: 0)
 0: Spindle brake on
 1: Spindle brake off
Cycle run
1
Moves to the starting point at rapid traverse, depending on RB:
 RB not programmed: Moves up to the safety clearance
 RB programmed: Moves to the position RB and then to the
safety clearance
2 Drills at reduced feed rate (50%).
3 Moves at feed rate to end of hole
4 Retraction at rapid traverse or feed rate, depending on D.
5 Return position depends on RB:
 RB not programmed: Retraction to the starting point
 RB programmed: Retraction to the position RB
Hole pattern: NS refers to the hole contour, and not the
definition of the pattern.